just a Word of Warning

[mayday]

from MPmaster post, line N10 WILL cause a crash under the right curcumstances ! for instance if you start the program and read the G43 tlo line, stop the machine with a reset, and then restart the program it will read line N10 and send the spindle into the part because of the G00 and G49 TLO offset cancel . we did not crash but caught it in time. this happened on a 15M Fanuc and also on a M32 Mazak control. I suggest removeing G00,G40,and G49 to stop this.

 

 

O0000 (TOOLPATH GROUP 1)

(PROGRAM - TOOLPATH GROUP 1.txt)

(DATE - APR-28-04)

(T1 = 5/8 SPOT DRILL )

N10 G00 G17 G20 G40 G49 G80 G90

N20 (SPOT FRONT PLATE)

N30 T1 M06 (5/8 SPOT DRILL)

N40 (MAX - Z.1)

N50 (MIN - Z0.)

N60 G00 G90 G54 X32.7558 Y-1.252 B0. S800 M03

N70 G43 H1 Z.1

N80 G99 G81 Z0. R.1 F2.5

N90 X39.4487

N100 Y-16.7519

N110 X32.7558

N120 G80

N130 G91 G28 Z0.

N140 G90

N150 M00

N160 M160

N170 M30

%

[Teh Bear without Brains kinda idiot]

Mayday !

 

I know machines that do need this (my machines do not )

Those who need can put skip line before /N10

 

But I think 99,9 % do not need this supersecurity and must take off this line

 

I never use restart ,anyway and do not use MPmaster .

So everyone must take his own decision .

 

God save you and your machinists from crashes .

I wish you safe machining ,

[specv]

Mayday

this is a standard safety line, if for some reason you forget to turn cutter comp off at the end of another program and run a program without this line you could be in a world of hurt. I think you should teach the operators what they need to read and what they do not. This is like saying that if you dont have a tool length offset that it will crash, obviously. Operator should always read the tool length offset as when you reset it clears out the tool length.

[Code_Breaker]

Mayday,

 

Just curious . . .

 

Where do you pick up your tool offsets? The reason I am asking is that you are drilling to Z0. with a rapid plain at R.1. Is this just an example or actual code? All of these are non-movement code, except G00. When the G49 is called, does your method to taking tools offset cause a movement here?

 

The last company I worked for used this line before and after every tool call. The machine was a Fadal. It was used a a protection block and was very effective.

 

Code_Breaker

[mayday]

quote:

---

if for some reason you forget to turn cutter comp

---

its not the dia offset that will cause this, its the tool lenght that will !!!. again just a warning. in our case a machine with 75in of ram travel with a tool lenght offset of say 30". if you stop the Z and only jog clear the ram any less than the tool lenght offset value,your gonna find the part in a not so nice way when restarting the program cause the G00 G49 will cause the Z to move to the previous Z position without comping for Tool lenght

 

 

quote:

---

Is this just an example or actual code?

---

yep, just a quick output

[specv]

maday

when our machines are reset the tool length is lost, as soon as you hit reset. not only when you read the safety line they are the fanuc pro3 control (18m)

[specv]

double post

[mayday]

Where it really got us was on the Mazak. the guy wrote a main program in Mazatrol to drill and index on a haas indexer. then he called the subs that I wrote. the machine was at retract position over the part after drilling in Mazatrol. so when it read the first line in the sub it was told to cancel Tool lenght comp. so it wants to send Z down. Not looking for arguments as to When,How,Why,Where. Im just stating it can happen.

[Guest CNC Apps Guy 1]

Users of AICC/SHPCC/HPCC have to have a G49 before each tool change because the machine will fail to run on the second toolpath if does not cancel the G43 for some reason. You just need to train you operators where, when , how, and why.

 

JM2C

[Tim Johnson]

Can you add a g28 or g30 home callout before the start block? This would eliminate the problem and not add movement except for a restart.

 

N10 G30 (G28) Z0

N20 G30 (G28) X0 Y0 (FOR HORIZONTALS)

N30 G00 G17 G20 G40 G49 G80 G90

N40 (SPOT FRONT PLATE)

N50 T1 M06 (5/8 SPOT DRILL)

N60 (MAX - Z.1)

N70 (MIN - Z0.)

N80 G00 G90 G54 X32.7558 Y-1.252 B0. S800 M03

[Allan Brown]

How about a retract G28G91Z0(G49?) prior to the saftey line as a way to satisfy all?

[Mike Whitten CAD/CAM Contractors]

That is what I always do. Also, you can just search for a tool and hit "go" regardless of "Z" position.

 

Mike

[Phil Orenstein]

To avoid crashes, (becuase I had too many) I would change the lines:

N70 G43 H1 Z.1

N80 G99 G81 Z0. R.1 F2.5

to:

N70 G43 H1 Z2.

N80 Z.1

N90 G99 G81 Z0. R.1 F2.5

Then I would single block it, lower the feed on the override and watch the dist to go page!!!

Mucho safe!

 

Phil

[mayday]

I simple changed this

N10 G00 G17 G20 G40 G49 G80 G90

 

to this

N10 G17 G20 G90

 

in psof of the post

 

pbld, n, *sgplane, *smetric, *sgabsinc, e

[specv]

what i was trying to say maday is that you should at least leave the G40 in there. if cutter comp is active and you run a drill cycle it will comp the position of the drill. this can be very bad. i have also seen a couple of tenths shift in some holes and could not figure out why the location was off.

[TheePres]

Bad experience with "G49" here also, working on older Fanuc 6M controls. Standard practice now to delete from Post.

[Roger Peterson]

I have seen machines do this, not good. Personally I would leave the G00 and G49 in and add a Z0 to the safety line. Because you never know where you are at during a restart this will bring you all the way up. During normal operation chances are your Z went all the way up at the end of the program anyway so it shouldn't cost you any time.

 

 

JM2C

[Mgrenier]

Mayday,

 

We have the same problem with our Fanuc controls. What we did is just remove de G49 as this is the only code that will cause any problems.

 

Just my 2 cents,

[Guest CNC Apps Guy 1]

It depends where you call the G49. If you cal;l it at the end of a toolpath, it could very well slam. I call it right after a tool change so I do not have problems with it.

[specv]

our G49 is in the tool change program itself. i know we didnt put it there.

[Dave Loveridge]

We never use the G49 it has caused crashes here too, and we have never found it neccesary to cancel offsets, we just load the next set of offsets and continue on.

[Reece L Gibson]

Thats the same thing I do Dave, I never use "G49"

If you think about it, "M06' is what really returns Z axis to the tool change position on most machines.(Some use "G30")Key in M06 by itself in MDI and see where it goes.On twin arm machines it just swaps the tool with who ever is in the ready position.On the older machines it calls a macro that does the tool change.Macro's can be called by M codes of you choice.Create your Own "G" codes as well.Each machine is different, they can set what they like at the factory.

[Allan Brown]

You know, we don't cancel G49 anywhere else, we just recall G43, so I'll yank it out.

[heeler]

I was taught to always return the machine to Z home when starting/restarting any machine. It would seem to me that there are certaing things an operator should know/do all the time. Knowing how to make the machine run and how to avoid certain problems would be most important. I also use the single block and read the distance to go all the time. I have to run programs that lots of people have written and some of them love to change things without knowing what they really do. Also on some older Fanuc controls you will get 2 tool length offsets applied if you don't cancel the first with the G49.

 

JM2C

 

Glenn